Popping and rough edges aluminum 1/8"

Hi all,
I am relatively new to CNCing, at least with the Shapeoko Pro 5 with a VFD. I am cutting 6061 aluminum McMaster-Carr (89015K68) using a YONICO 1/8" 0-flute (#31012-SC).

I am running at 18,000 RPM, plunging at 3, feeding at 15, and depth per plunge at 0.015. (I hope those units are self-explanatory.)

In the last few weeks I have used the exact same set up and all has worked great. But I just received a new 2x4’ sheet of the 6061 and started cutting and it has been rough. I am getting frayed edges for any diameter whole and some knocks and pops I have never heard before. It was worse when I had the feed and DPP higher so I brought them down to the levels noted above.

I also did some cutting without the vacuum, and the VFD is very quiet, so I have ruled out bearings. (it is only 6 months old and is used only weekly for a few hours. )

It is a 14 hour cut and I am monitoring it. All seems to be going according to plan but the knocking, popping and frayed edges are unique.

Could it be bad aluminum? Any other ideas? I have offered a picture and a short video.

Thanks, in advance, if anyone has any ideas.


video link: https://photos.app.goo.gl/CMWTuVbE15y7fdBZ9

How old is the endmill?

I cut quite a bit of thin aluminum sheet and have had better success going with a shallower doc, .01 or less, and really bumping up the feedrate. Im sure others may disagree with that approach but it works well for me. You could also run a chamfer pass to clean up the edges, even with “perfect” settings i find a little clean up is usually necessary.

end mill is brand new.

A chamfer pass is not something I considered. Good idea.

Any ideas on the odd knocking and popping?

Generally, I’d look at chip evacuation for the knocking and popping. (If I’m imagining the sound right). Maybe a little air in the cut to help clear?

I’ve read a lot about China aluminum being unpredictable and with strange hard spots and uneven cutting. We always specify US aluminum if it’s available so we haven’t seen that personally.

Finally, I’d look at the cutter through a loupe. One bad cut, or recut chip, and the flutes could be damaged. I don’t know YONICO, but it sounds like a China vendor and I’ve been told (by US tool vendors) that many China tools use a lower grade of carbide with larger grain size. I don’t know if that’s true, or if that can lead to easier breakage.

1 Like

Those sounds can be heard right at the end of the video.

@wmoy Is on a much-needed vacation but he might be able to chime in on speeds and feeds. Those seem conservative to me, but it’s been a while since I cut aluminum on a Shapeoko.

And sorry I missed the mention of McMaster for aluminum. I’d be shocked if the aluminum from them varied much.

1 Like

Sadly, I am not actually on vacation, but the good news is I don’t hear anything too concerning from the cut. Usually you get some small shrieks in direction changes or cutting into corners as the forces shift rapidly on the endmill. And sometimes at the start or conclusion of plunges or ramping moves there can be a little chirp as the CNC freezes for a couple milliseconds.

The vacuum does help, though it’s not as good as a stream of compressed air. But for shallow cuts it should still be sufficient.

I don’t know what you’re doing your toolpaths in, but if you have the control to set your cutting direction to “Climb” or “Left”, your CNC will have a slightly happier time when cutting.

And I’m personally with Chris in that a lot of times, I’ll prefer to cut shallower but faster unless I’m using a fancy toolpath like Fusion 360’s Adaptive. You likely can also crank up your RPM as well and increase the feedrate proportionally.


Really interesting. I had seen some strange hard spots. Check out the things that are circled here.

And the bit broke. I am doing some countersinking to inlay some numbers and it did not like that. I gave up for the evening and came home without getting a picture of the last number path. The edges got really frayed and then it snapped. Ill post one tomorrow.

I did get all the screw holes and bearing holes done. (This is for a robot chassis.)
So tomorrow I can switch to a 1/4 to get the pocketing done and get the pieces cut out. Hopefully that can stand the stress.

But the bad aluminum sure feels right. Every other time things cut like butter. This was shockingly loud, and all the crackling and popping made me think the metal was very brittle.

(as a new user I can only post one picture)

other pics

I’ve upgraded you — hopefully that will help.

I’d definitely contact McMaster-Carr about this and send them those photos.

1 Like

Thanks wmoy. I am using Carbide Motion. Does that have Climb and Left? Thanks for the advice on the shallower cuts. How fast do you suggest we run the VFD at? And if we were to increase it by 50% do you suggest increasing the feedrate by 50% too?

Regarding the vacuum, it is a Bosch with 150 CFM (https://www.boschtools.com/us/en/products/vac140ah-06019C3511). Its a beast. I have actually kept it at a lower CFM than that because it will draw pockets right off the tape-down material and can get caught in the bit. But it has had no issue clearing the tool path.

No, Carbide Motion only sends G-code, and the G-code implementation lacks the features for reversing things (assuming that’s even possible in G-code).

Carbide Create doesn’t have a native facility for this either (though one can trick it using offset contours).

Sorry. I got myself confused. We use Carbide Create (at least for now).

And here is what it looked like before the bit broke. the lower part of the picture is the number it failed on.

FYI I have doing some more reading on “bad aluminum” and found another discussion here:Shop Management and Owner Issues | Poor Quality Aluminum Sources | Practical Machinist - Largest Manufacturing Technology Forum on the Web

I would be curious if folks had advice for sources other than McMaster-Carr that folks have used for single 2x4’ sheets. the Multipurpose 6061 Aluminum Sheet 1/8" Thick, 24" x 48" sheet we bought says it should have a “Material Certificate with Traceable Lot Number”. I’ll have to look for that.

I called just now and they said they would “check the stock for quality” and send us a replacement. I am kinda amazed at that service. But I wish they had just “checked stock” before. (They are also throwing in a new endmill)

For hole milling with a 1/8" O-flute in 6061, I use 12000 RPM, 20 IPM, 0.005 DOC (Depth per revolution on the helix), 0.030 stepover, with mist coolant.
I also use climb cutting, which can be a challenge in CC. You have to offset your curve, use contour with no offset, ramping, and mirror the curve to flip the direction of cut.

The pics show melted material which 9/10 times is either too low of a feed rate or chips are not clearing out and getting recut. It could very well be inconsistent material, but I’m more likely to think too low of a feedrate and lack of chip evacuation. Air blast kits are really affordable and help a lot on plastic and aluminum. On areas you’re not cutting thru, a little bit of mist with cutting fluid or isopropyl alcohol will help even more.

I’d start with reducing depth of cut and increasing feedrate. I also tend to use high quality, coated bits. Carbide 3D and Amana are my go-to vendors. Then get you an air blast kit to get those chips out of the cut and keep them from causing trouble.


Thanks SLCJedi. Great info. Regarding air assist, we had planned on doing that initially.
We have been running for 6 months and cut a ton and never had this problem and we are in a school classroom without a cover, so blowing the bits is not the preferred solution. So we went with the bosch and have never had an issue.

The 2nd number is where the problem started occurring as the bit was failing. Does it appear like there is melting on the 6? (Again, we have cut these numbers out 2 other times and never had an issue.) But, we did decrease the feed rate and given all these comments I now understand that comes with some risks. The metal can heat up and melt if the rate is too slow. I had not understood that.

Anyway, we believe either this is not 6061 (it was screwed up at McMaster-Carr and they inadvertently shipped us the wrong thing) or it was but it was cheap Chinese stuff.

1 Like

Ben, there are a number of things that can go wrong with cutting aluminum. We are not guaranteed that the material is of solid aluminum at the grade you want. Sometimes, if the company making the aluminum allows of materials get into their melts, then the aluminum could become harder in those areas. Also, aluminum shavings need to be removed from the cutting area as the cuts are being ran. If aluminum shavings are not removed from a cutting area effectively, the shavings will tend to get hot and melt themselves together, stick to the endmill, and cause poor cutting or even breakage of the endmill.

Aluminum can be cut very aggressively, but it is important to keep the material cooled down and the chips removed properly. I have cut aluminum in all different sizes and depending on the types of cuts and the sharpness of my endmill, will determine the cleanliness of my cut edge. Heat is your enemy when it comes to aluminum. It gets hot and melts easily another. Some holes that might be cut with a drill for relief should be done beforehand.